Re: [CAD_CAM_EDM_DRO] Using a tapping attachment with a CNC bore cycle

"Fitch R. Williams" wrote:

> On Fri, 15 Feb 2002 06:38:16 +0000, Jon Elson <elson@...>
> wrote:
>
> >I just used the RPM as stamped on the milling head nameplate, plugged it
> >into a formula, and used that for the feedrate. It worked superbly, and the
>
> So you are tapping at 1,000 rpm or more? Eeeeeee Haaaaaa! Cowboy Up,
> Hang on and nod. Is there a buzzer after 8 seconds? <G>

Nope. If I had a little more acceleration in my machine, I would probably
try it. I Think I might do it at 660 RPM, though. I don't have one of the
programs handy to check what speed I used.

>
> A 1/4-20 tap at 1,000 rpm would require a feed rate of 50 in/min. My
> mill has a max feed rate of 40 in/min so I think I'll have to reduce the
> rpm. I was thinking of tapping at more like couple hundred rpm. Should
> I be planning to tap at as high an rpm as I can and still be within the
> feed rate constraints? That's a scary thought at the moment. I do
> nearly all steel. I've been tapping at 80 rpm in the manual mill - my
> aging reflexes aren't up to anything faster. I need to free myself from
> the constraints of manual machining for tapping?!?

Due to the acceleration needed (and deceleration at the bottom), I'd
go about half speed, unless you are in a hurry. Most of my tapping has
been in Aluminum. Depending on the steel, type of tap, etc. you will have
to decide what RPM sounds right. For 20 IPM plunge, and 20 TPI, that
would come out to 400 RPM. I don't know how hot a tap will get at
400 RPM in steel, but it will be a lot hotter than in aluminum.

>
> OK, tooling update (gloat?). I just bought another tapping head on
> Ebay, a Tapmatic N/C R-1, that goes from #10 to 1/2", new in the box,
> for 27% of its new cost. See
>
> http://cgi.ebay.com/aw-cgi/eBayISAPI.dll?ViewItem&item=1702558223
>
> if your interested. Sort of excited about this one - I do a lot more
> holes in the #10 to 1/2" size range. The NMTB40 adaptor fits The
> Animal.

You'd better check the spindle HP requirements before tapping a 1/2 - 13
hole in steel with a tapping head.

> Anyway, I am going to be machining a couple of aluminum blocks to make a
> coolant pipe fixture for my lathes (and for the manual mill) that will
> have some tapped holes including two with 1/8"npt. (The aluminum block
> for use on the lathes will bolt to the top of a real cheap import
> magnetic dial indicator base replacing the useless plastic block that
> came with it.) I could hand tap the pipe threads but might just
> experiment since that is in the size range for the new tapping head, and
> there will be two such holes side by side - the vary thing CNC machines
> are supposed to be good at. I'll machine some air and make sure the
> depth is right on before going for the chips.

I don't know if you can do pipe taps with the CNC head, unless you use
the tapered reamer, first. The pipe tap starts out real shallow, and then
gets deeper and deeper, drawing more and more torque.

>
> >only 2 taps I've ever broken with it were caused by feeding too DEEP, not
> >by feed getting ahead of the spindle revolutions.
>
> I hear the too deep. That concerns me also. Since the CNC tapping
> attachments don't have a torque relief, that requires careful thought
> when setting up the program.

And, making sure the hole is really drilled as deep as it was programmed.

Jon